When using the Linear Sketch Pattern it will fail when I enter a distance greater than 12". Up to 12" it will work, but any distance larger that 12" and the feature fails to execute. A window appears with the message: "Please enter a number between 0 and 3280'-10 1/16". Has anyone run into this issue and/or knows a solution to this? Please see attachment.

Out of curiosity are you patterning features or bodies? When you are patterning independent bodies like you have seemingly shown, I find that patterning features becomes hit or miss so I always by default pattern bodies when I can....

I can pattern it both X and Y directions for distances 12" or less. If I go above 12" I get the message pop-up and the command will not complete. I can't post the part right now because I'm at work, and curiously it works fine on the work computer (version 2014). I have two laptops at home, one loaded with 2014 and one with 2015. The feature fails on both of these computers.

Okay, Dennis got me thinking when he mentioned the hyphen in the dimension. So I have discovered two things. In 'Document Properties > Units' I have my default set to 'Feet & Inches', and this seems to create the glitch. If I change the units to 'Inches' like the SolidWorks Part default, it works perfectly. If your 'Units' default is 'Feet & Inches' the work around is to enter a distance of less than 12" in your Linear Sketch Pattern and toggle on 'Dimension X and/or Y spacing'. Then select the dimension in the graphics area and you can change the value to whatever you want and the feature builds correctly.

Or you can change your 'Units' to 'Inches' in the 'Document Properties' and the feature will also work then.